SOLIDWORKS Drawing templates contain all the document specific information that is found in the Tools > Options > Document Properties dialog (i.e. units, standard, fonts, arrow sizes, etc.). SOLIDWORKS Sheet formats contain the Title block information as well as the information from the Sheet Properties dialog.
When saving a drawing template, the sheet should be empty (even if the sheet format is deleted from the Feature Manager).
To save a sheet format, when it is displayed go to File > Save Sheet Format.
If you do not want to have the default sheet formats available when creating a new drawing, one of the following requirements must be met:
The popup dialog of sheet format/size depends on the type of the drawing template.
Open the DWG file in SOLIDWORKS. Highlight the entities that will make up the sheet format by selecting them using a selection box. Hit CTRL+C to copy the selected entities. Create a new drawing. Right-click in the drawing and select Edit Sheet Format. Delete any existing contents and hit CTRL+V to paste the DWG contents into the SOLIDWORKS sheet format. Go to File > Save Sheet Format and save the sheet format as a .slddrt to be used in other SOLIDWORKS drawings.
The drawing template needs to be saved without any sheet format in it. This will cause the user to be prompted to select a sheet format when making a new drawing using that template. To accomplish this, right-click on the Sheet Format in the design tree and select Delete; then save the drawing template.
This can be easily achieved by simply changing the sheet format after the sheet has been added to a drawing.
Right-click the Sheet Name in the feature tree, select Properties. In the Sheet Properties dialog, browse to and select the desired alternate sheet format.
The type of projection and the other sheet properties are not saved in a sheet format; they are saved in an individual drawing file or a drawing template. Sheet formats can store linked custom properties, title block information, anchor points, and OLEs.
Predefined views cannot be saved in sheet format. By design, sheet formats cannot hold drawing views. They can only contain sketch entities and annotations.
Unfortunately, a Revision Table cannot be saved to a drawing sheet format. A revision table can only be saved to the Drawing template.
Check Tools->Options->System Options->File Locations->Show Folders for. Sheet Formats and make sure that it is pointing to the location on the hard-drive where the sheet formats are located.
The default location for drawing sheet formats is:
Windows® XP: C:\Documents and Settings\All Users\Application Data\SOLIDWORKS\\lang\sheetformat
Windows Vista®, Windows® 7: C:\ProgramData\SOLIDWORKS\\lang\sheetformat
It is possible to change the location, from the main menu -> Tools -> Options -> System Options -> File Locations -> Sheet Formats.
A drawing template can be saved with or without a sheet format. A new drawing created from a template that does not include a sheet format will prompt for a sheet format when a new drawing is started. A new drawing which does include a sheet format will simply display the stored sheet format. In this case, when adding a sheet, SOLIDWORKS will search the path where the original sheet format was located when the template was saved. If the sheet format is no longer at that location, then there will be a message when adding new sheets. To correct the problem, re-save the drawing templates with the current sheet format paths or simply remove the sheet format from the template.
To resolve this:
To accomplish this, include a drawing view of the model with the desired custom properties. You can then access those properties when creating linked annotations. The drawing view will not be included when you ‘Save Sheet Format’, but the linked annotations will retain the correct source-property information.
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